Seemingly simple constraints in an assembly being impossible to implement

Spring 8K Slipper 1.zipHello, thank you for taking the time to read my problem.

I'm learning Inventor. As I often do when learning something I come up with a project I want to do and learn as I complete the project. In this case I've decided to design a dump trailer which I'll actually build. I've been doing well with most constraints and piece placement but I'm having fits trying to build the leaf spring assembly.

I did all the profiles in AutoCAD (yes, I've been reading other posts and the consensus seems to be to use the Inventor sketches and I'll learn that better later; right now I am only doing some of my drawings as sketches in Inventor). The curved leaves are concentric and have uniform radii. I've attached (or will, I should say) my assembly file and the individual leaf files.

Basically I've modeled the leaves of a leaf spring assembly including the alignment/retainer bolt hole at the middle of each leaf which I use to help assemble the parts in Inventor. The first thing I try to do is, using Assemble, choose Mate-Mate to put the top of the lower leaf to the bottom of the upper leaf. That keeps the leaves from being mobile along the Y axis as orientated when it is in proper position in the real world. I then make the narrow side flush across the leaf I'm working with to the one above it. That makes sure the leaves are all in a neat stack with even sides and that they cannot pivot/rotate around the axis of the alignment hole, for example. Finally I need to constrain the leaf so that it cannot rotate as viewed from the side either clockwise or counterclockwise. So here I constrain with Mate-Mate the axis of the lower leaf alignment hole to the axis of the upper leaf alignment hole.

This works well to lock the pieces together where they are supposed to be but I cannot assemble the entire stack of six leaves. I've tried this for hours and the most I can achieve in a stack is 4. I'm sure that I'm doing something fundamentally wrong but I don't how to put the question in to words to try a search. I read through some posts here but finally just decided to post this.

Thank you for your time.

--HC

Spring 8K Slipper 2.zip

OK, I went through this assembly - and this is a very good example of why you should start over from scratch in Inventor rather than using AutoCAD.

Not that there is anything wrong with using AutoCAD, but rather, a lot of what you did in AutoCAD is wrong.

Do one part in Inventor from scratch and attach the *.ipt file here.

Once I explain how you should have done the part (based on how you do model it), the design will go very fast.

"I'll learn it later" is NOT the way to go about dealing with Inventor's sketch environment. Sketches in Inventor are the absolute most basic building block. If you don't take the time to learn how to do them, and do them correctly, everything you do afterwards will almost invariably be done poorly.

OK, I went through this assembly - and this is a very good example of why you should start over from scratch in Inventor rather than using AutoCAD.

Not that there is anything wrong with using AutoCAD, but rather, a lot of what you did in AutoCAD is wrong.

 

Do one part in Inventor from scratch and attach the *.ipt file here.

Once I explain how you should have done the part (based on how you do model it), the design will go very fast.

JD, thank you for taking the time to look over my drawings and problem.

I've re-done one part in Inventor entirely. I had to use AutoCAD to get the numbers I needed to do the sketch; is that normal or is there some way I should be able to use sketching in Inventor to determine the numbers?

Regardless, the one part (top leaf of the spring assembly) has been re-created and I'm attaching it.

Not being rude or offended; I would ask what I did wrong in AutoCAD? If I'm doing something wrong I'd like to know so I can try to correct it.

Thank you again for your help and time.

--HC

SpringLeafinInventor.zip

"I'll learn it later" is NOT the way to go about dealing with Inventor's sketch environment. Sketches in Inventor are the absolute most basic building block. If you don't take the time to learn how to do them, and do them correctly, everything you do afterwards will almost invariably be done poorly.

Fair enough, but I have been trying to do what I can in Inventor sketches and only reverting to AutoCAD drawings when I felt I had to, like trying to determine arc radii for subsequent leaves of this assembly. I had not gotten the idea that using AutoCAD drawings in Inventor was synonymous with flat doing it wrong. It is not my intention to have a bad attitude towards this or come across that I do.

--HC

I am going to walk you through this showing you some techniques that are actually more advanced than I would like to introduce on a beginning project, but I think you will figure out why as I go along.

First of all, your Inventor dimensions don't match the AutoCAD part sketch that you posted earlier.

Second, some of the dimensions in the AutoCAD part sketch and in the Inventor part are not manufacturable.

Start a new part file.

Expand the Origin folder in the browser and make the Center Point visible (right click on it in the browser).

Create the sketch shown below (horizontal line is construction line type (right click or upper right corner of screen to control) and the circle at origin is dimensioned as a fraction (don't do calculations - this introduces errors, let Inventor do the math.

Attach the file here.

Circle and line for JDMather.iptHello, JD, thank you for the reply. I'm sorry for the delay; I don't get to work on the projects I want to every day.

I've gone back now several times and re-done my drawings in Inventor, getting a little better at the sketching. I just completed all six parts from scratch last night and tried to stack them and got the same kind of errors I got when I was using profiles from AutoCAD. I won't bother to post them as it seems unnecessary (unless you ask for them) since, from the example you're working me through, it seems what I'm missing is really fundamental. Thank you for taking the time to help me.

I did the sketch you asked for and am attaching it. I don't mean this to give you any grief but I would like to understand what the difference is between entering 1.1875 and 1-3/16"? The obvious difference is, to me, that occasionally I do something boneheaded like use 0.3125 for 3/16, which I did recently in a drawing; entering 1-3/16 eliminates that kind of brainless error.

Anyway, thanks again for your help.

--HC

I would like to understand what the difference is between entering 1.1875 and 1-3/16"

There is no real difference in most cases, but there are two possible scenarios where it does make a difference.

1. user inadvertently transposes digits (you indicated that one)

2. a stackup of fractions (particularly if the user rounds off the true value, which is a common occurrence) could result in position calculations not matching up exactly in the assembly.

I normally enter the decimal equivalents if I know them, and they don't go out too many decimal places - otherwise I let the software do the calculation.

I'll be back in a bit. Add these two lines at the right end of the construction line.

Notice how I have edited the offset dimension from the end of the construction line and given it the name Thickness.

The big thing about using the fraction there is that it's a demonstration of a useful concept: Inventor can do math for you in dimension boxes. You can enter pretty complex equations in there, and Inventor will figure it out for you.

Now edit Sketch1 and create the arc as shown.

Note that there is a Tangent constraint to the circle on the left.

Note that there is a construction line drawn from the center point of the arc Vertical trimmed to the arc (the second end is not at the midpoint of the arc).

Dimension the distance from the horizontal construction line to the intersection of the arc and the vertical line exactly as shown (this will eliminate first source of problem in your previous attempts). After attaching I see that box isn't real clear. The dimension is 3.5+Thickness.

Edit Sketch1 and add the 50° construction line from the center of the circle on the left as shown.

Trim the arc.

Exit Sketch1, right click on Sketch1 in the browser and turn off visibility of the Dimensions (for clarity in the next steps).

Start a new Sketch2.

Project Geometry the large arc from Sketch1 (your sketch won't look any different since the projected line is overtop the original).

Offset the arc as shown and dimension the offset distance.

Project Geometry the vertical line from Sketch1

Create an angled construction line from the end of the projected vertical line (the centerpoint of the arc) to the end of the arc on each side.

Add a Symmetry constraint selecting the two angled lines and then the vertical line. Dimension the angle.

Repeat for each spring leaf with desired angle. (or you could dimension arc length or chord length - whatever is the known, driving dimension)

Attach the resulting file here.

The next step will be the "trick". (1 of 2 tricks)

The big thing about using the fraction there is that it's a demonstration of a useful concept: Inventor can do math for you in dimension boxes. You can enter pretty complex equations in there, and Inventor will figure it out for you.

Okay, got it. Thanks for the explanation. I'll have to see some examples (I have a book I'm trying to work through but one of my shortcomings is tearing off on things) to see how it might benefit me. I can see where this would probably be helpful when one names the driving dimensions (in the book I read that we can name a dimension) so one could name the length "Length" instead of "d2" or whatever, then reference that in another dimension such as, "=Length/2" (the syntax may be wrong but the gist is there).

Thanks again.

--HC

Circle and line for JDMather rev 2.iptJD, thank you for your time (again and always).

I've gone through the steps you've outlined and I think I've followed everything. I'm attaching the file.

--HC

Look in the browser at Sketch1.

Notice that there is not a thumbtack image on Sketch1 like there is on Sketch2.

This means your Sketch1 is not fully defined.

Edit Sketch1 and notice in the lower right corner of the screen it says that 1 dimension is needed to fully define the sketch.

Actually constraints or dimensions can be used to fully define sketches - I use constraints over dimensions depending on the design intent (what might change).

You have left a dangling endpoint on the end of the 50° construction line.

Does this effect the geometry. No. But in my opinion it is critically important for a beginner to fully define every sketch.

Simply drag the endpoint of that line up to the endpoint of the trimmed arc.

As you get more experience with Inventor and learn how it creates geometry constraints - Inventor will do this work for you, so right now you might consider it to be extra work, but it will be automatic as you get experience and will save you extra work down the road.

I thought is was sort of implied in previous post that you would continue on offsetting the arc 3 more times for the leafs of the spring (see attached image). (you can ignore the yellow dots in my image - simply means that I left the display of the constraints visible (which I normally don't do))

Here is image of my two finished sketches with dimension display turned off. I normally don't turn off dimension display unless the dimension are set in stone (won't change). If a dimension does need to be changed it is a simple matter of double clicking on the dimension.

I could have eliminated all but one of the Thickness dimensions by using short vertical lines from the end of the original vertical line and then making them Equal (=) constraint. That is what I would normally do for something like this. This would be a good challenge for you to figure out (actually pretty simple).

Extrude each sketch midplane (symmetric) 2" (because the profiles are open you will have surface bodies.

After doing the second Extrude you will have to expand the ExtrudeSrf2 feature and right click on Sketch2 and select Visibility.

After extruding the surfaces then Thicken each one by Thickness (for the first Thicken set to Quilt since it is multiple surfaces).

Be sure be sure be sure to set as New Solid for each Thicken (after the first one).

Right click on the Surface Bodies folder in the browser and turn off Visibility.

Add you fillets to each solid body.

Turn the visibility of Sketch1 back on and start a new sketch on the XZ Plane.

Select Project Geometry and then the vertical line from Sketch1.

Add a (sketch) Point at the projected point.

Hit H on the keyboard to start the Hole command.

Select all of the solid bodies to drill holes Through All.

Set you desired hole diameter.

Turn off visibility of the Sketch1.

Post back for instructions on how to convert this multi-body solids file to an assembly if desired.

I'm following along with this tutorial also because I am lacking in the basics of all cad really. There are certain "faults with my Sketch1 that I can't seem to resolve, I used sketch Doctor to identify them but I'm still not getting anywhere. Before I progress any further I would like to drum into my thick skull the correct way of working as best as I can.

I'm attaching my file.

It tells me that Sketch1 needs 3 dimensions that that there's an open loop, but I can't seem to get the loop closed, the construction line gets in the way.

If you feel that I'm being inappropriate in asking/high jacking this thread then just ignore me.

I'm using Inventor Professional 2014 Student Edition.

Part1.ipt